[nusivares]

Hi,

I am in my Friday afternoon fury.

I have spent the whole afternoon googling about with no result on a fairly simple problem.

For some strange reasons there is very little documentation on how to sample a fixed size square plane through the domain.

It should be very easy and a standard thing to do. But it is not.

And I do not want to press a bunch of button on paraview every time to get the surfaces out. I would like a simple script. The code below does not cut it. Just produces the slice through the whole domain which further annoys.

I checked the points and the points are ok.

Essentially I want to limit my plane by those 3 points.

type surfaces;
libs ("libsampling.so");

interpolationScheme cellPointFace;

surfaceFormat vtk;

surfaces 
(
    xNew
    {
	type            cuttingPlane;    // always triangulated
	planeType       embeddedPoints;
	embeddedPointsDict
	{
	point1		(0       	  0.0005    0.00407);
	point2		(0.00125          0.0005    0.00407);
	point3		(0                0.0014    0.00407);
	}
	interpolate	true;
       }
)

[akidess]

Use an STL sampledSurface.

[nusivares]

Hello,

Do you have an example syntax of it?

Cannot find it in .H file or anywhere within the bound of Google.

[nusivares]

Anyone? I cannot find any examples anywhere of a such thing.

[ykanani]

Hi,
I believe you can use faceZone sampling. You need to define a faceZone reflecting the surface that you need to sample. To do this, run setSet utility. First define a faceSet. you can type help to see the syntax. Then, create a faceZoneSet based on the faceSet that you just defined. So it will be something like this:

run this command, then you will be able to run the following commands

setSet

after running setSet:

faceSet f0 new boxToFace (0 0 0) (0.1 0.1 0)

hint: change boxToFace to something like "apple" and run it, openfoam will show you options that you can use instead of boxToFace to define your surface.

Then, convert the faceSet to faceZoneSet:

faceZoneSet f0Zone new setToFaceZone f0

and quit:

quit

Now that you have defined the faceZoneSet, add this to the controlDict file under functions:

YourDesiredName
    {
          type            surfaceRegion; //for of4.1 //surfaceFieldValue //for of5.x ;
          libs            ("libfieldFunctionObjects.so");
          surfaceFormat   vtk;
          writeControl    adjustableRunTime;
          writeInterval   1e-03;
          writeFields     true;
          log             true;
          regionType faceZone;
          fields          (U p);
          orientedFields  (phi);
          operation       none;
          name    f0Zone;
    }

Note: use surfaceRegion for OpenFOAM 4.x and surfaceFieldValue for OpenFOAM 5.x. I tested this in OpenFOAM 4.1

You can use your preferred output intervals by editing the write method (specified in red). You will find vtk files under postProcessing/YourDesiredName/surface folder
Please take a look at the following files for more information and examples:

OpenFOAM-5.x/etc/caseDicts/postProcessing/flowRate/flowRateFaceZone
OpenFOAM-5.x/etc/caseDicts/postProcessing/flowRate/flowRateFaceZone.cfg
OpenFOAM-5.x/etc/caseDicts/postProcessing/surfaceFieldValue/faceZone.cfg
OpenFOAM-5.x/etc/caseDicts/postProcessing/surfaceFieldValue/surfaceRegion.cfg

You can find the detailed explanation in the header files:
OpenFOAM-5.x/src/functionObjects/field/fieldValues/surfaceFieldValue/surfaceFieldValue.H
OpenFOAM-4.x/src/functionObjects/field/fieldValues/surfaceRegion/surfaceRegion.H

Hint: you can do various operations on the field you sampled as well, check the mentioned header files for details.


Regards,
Yousef

[nusivares]

Just leaving here two solutions: new OpenFOAM version has the feature called bounded plane. Alternatively, it is possible to do batch processing using paraview. It is a similar way of doing post-processing as with CFD post within Ansys suite. It is called tracing and creates a python script and can be accessed through Tools-> start trace. Here you record your operations within paraFoam. For sampling a limited size plane, this can be:

#### import the simple module from the paraview
from paraview.simple import *
#### disable automatic camera reset on 'Show'
paraview.simple._DisableFirstRenderCameraReset()

corrug_ALMcOpenFOAM = OpenFOAMReader(FileName='./core_ALM-channel-25.OpenFOAM')
corrug_ALMcOpenFOAM.CaseType = 'Reconstructed Case'
corrug_ALMcOpenFOAM.Createcelltopointfiltereddata = 1

# get active source.
corrug_ALMcOpenFOAM = GetActiveSource()

# Properties modified on corrug_ALMcOpenFOAM
corrug_ALMcOpenFOAM.CellArrays = ['T', 'alphat', 'p', 'p_rgh', 'U']


writeCuttingPlanes1 = True
if writeCuttingPlanes1 == True:
	# create a new 'Clip'
	clip1 = Clip(Input=corrug_ALMcOpenFOAM)
	clip1.ClipType.Origin = [0, 0.01, 0]
	clip1.ClipType.Normal = [0.0, 1.0, 0.0]
	clip1.InsideOut = 1

	names = ['x1/x1.vtm' , 'x2/x2.vtm' ]

	orig = [[0.005 , 0 , 0] , [0.0186 , 0 , 0]] 
        	
	for i in range(len(names)):
		slice1 = Slice(Input=clip1)
		slice1.SliceType = 'Plane'
		slice1.SliceOffsetValues = [0.0]
		slice1.SliceType.Origin = orig[i]
		slice1.SliceType.Normal = [1.0, 0.0, 0.0]
		SaveData('./postProcessing/cutPlanes1/'+names[i], proxy=slice1, Writealltimestepsasfileseries=1)
		print('Layer 1 = ',i )

Note: when you trace - there will be a lot of rendering lines left which could cause trouble - delete them, leave the lines left related to data extraction only.